[Schematic Review Request] STM32 WB Bluetooth Dev Board

[HasanSyr]

In addition to the entire schematic kindly take care of the following:

• TPS736 LDO:

I want to tie the EN pin to Vin however on page 14 on the datasheet it says:

7.3.3 Enable Pin and Shutdown The enable pin (EN) is active high and is compatible with standard TTL-CMOS levels. VEN below 0.5 V (max) turns the regulator off and drops the GND pin current to approximately 10 nA. When EN is used to shutdown the regulator, all charge is removed from the pass transistor gate, and the output ramps back up to a regulated VOUT (see Figure 19).

When shutdown capability is not required, EN can be connected to VIN. However, the pass gate may not be discharged using this configuration, and the pass transistor may be left on (enhanced) for a significant time after VIN has been removed. This scenario can result in reverse current flow (if the IN pin is low impedance) and faster ramp times upon power-up. In addition, for VIN ramp times slower than a few milliseconds, the output may overshoot upon power-up.

How can I ensure that V_EN is driven low before V_in? Can I add a delay like this https://imgur.com/a/f2qmQHG ? Does it matter at all?

• The DLF162500LT-5028A1 low pass filter is recommended in the application note (page 14) but I can only get 2450LP14A100T, is it a suitable replacement?
• Do I need to add any protections for I2C/UART/other pins?
• I'm using a 6-layer PCB (yes it's overkill), what stack-up should I use?
• I have a 1K Ohm resistor already for the LED so it doesn't matter for BOM consolidation.
• I'm going to create a PCB antenna so that's why there is no antenna connector.

https://imgur.com/a/VLBhM8H

[pcprogrammer]

I have no answers to your questions, but I see what I think is an error in your schematic.

You have the +3.3V power flag near U2 after the red led instead of before it. I guess that U2 is a 3V3 regulator (did not lookup the datasheet) since it is supplied from the USB VBUS pin, which is marked as +5V. Having the connection after the led means that the voltage will be the forward voltage of the led lower then the output voltage of U2. So 3.3V - ~2V = 1.3V.

I don't see the setup working that way.

[quadtech]

Check this thread

https://e2e.ti.com/support/power-management-group/power-management/f/power-management-forum/821665/tps73633-ep-overshoot-during-power-up-for-3-3v-fix-version

[Doctorandus_P]

Not a full review, but some notes:

• 3V3 power symbol on the other side of Led D1
• No capacitors on X1? (Are they integrated?
• Shorting C11 though the reset switch generates very high peak currents (10A or so) that destroy the switch over time. It's ok-ish for occasional use, but not if the switch is operated often. The high current can also offset GND levels. Add some series resistance, just like R5 for the boot0 pin.
• R3 is not OK. Apparently shield of USB must be directly connected to GND.
• The text "both caps 10pF does not work for the BOM.
• Add a programming connector.
• I prefer the PWR_FLAG for GND to be near the power delivery. Either connector or voltage regulator, not tugged away in a random location.
• I started putting PWR_FLAG symbols right on top of power symbols. I don't know whether I like that practice though.
• Circuitry around VLXSMPS looks unusual, but I have not checked with the datasheet.
• I place all decoupling capacitors habitually on the power regulator IC. This give a better overview (C1, C4 and C20 all 4u7?)
• For generic connectors, I prefer dual row connectors. Easier to connect to a breadboard, you can use a flat cable, or pull the wires apart and use them in bundles or individually).
• Mounting holes?
• Logo, project name, date or version number on the PCB?
• I don't like boxes around schematic sections, Whitespace works just as well.
• When a schematic has more sections, then make the titles for the sections "Power Supply" etc, bigger and fat. This makes them easily identifiable when zoomed out. It adds overview to the schematic.
• R1, R2, R4, R6. Si prefix for kilo is a lower case k.
• Why add a capital "F" to all capacitors, but no "Ohm" for resistors?
• GND pin for Rf module F1 seems to be stacked, (but stacked pins not hidden).  but you unstacked the pins for the uC?
• RefDes has standardized abbreviations. F is for fuses. https://en.wikipedia.org/wiki/Reference_designator
• I would prefer a few more Power and GND pins on the generic I/O connector.
• It looks like "VBUS" is not connected to: "VBUS (+5V)" (Both have a PWR_FLAG) In KiCad V8 the power symbol name determines the net name, and thus connections.
• I always prefer some kind of inductor or choke between the power input connector and the power regulator.

[HasanSyr]

Not a full review, but some notes:

• 3V3 power symbol on the other side of Led D1
• No capacitors on X1? (Are they integrated?
• Shorting C11 though the reset switch generates very high peak currents (10A or so) that destroy the switch over time. It's ok-ish for occasional use, but not if the switch is operated often. The high current can also offset GND levels. Add some series resistance, just like R5 for the boot0 pin.
• R3 is not OK. Apparently shield of USB must be directly connected to GND.
• The text "both caps 10pF does not work for the BOM.
• Add a programming connector.
• I prefer the PWR_FLAG for GND to be near the power delivery. Either connector or voltage regulator, not tugged away in a random location.
• I started putting PWR_FLAG symbols right on top of power symbols. I don't know whether I like that practice though.
• Circuitry around VLXSMPS looks unusual, but I have not checked with the datasheet.
• I place all decoupling capacitors habitually on the power regulator IC. This give a better overview (C1, C4 and C20 all 4u7?)
• For generic connectors, I prefer dual row connectors. Easier to connect to a breadboard, you can use a flat cable, or pull the wires apart and use them in bundles or individually).
• Mounting holes?
• Logo, project name, date or version number on the PCB?
• I don't like boxes around schematic sections, Whitespace works just as well.
• When a schematic has more sections, then make the titles for the sections "Power Supply" etc, bigger and fat. This makes them easily identifiable when zoomed out. It adds overview to the schematic.
• R1, R2, R4, R6. Si prefix for kilo is a lower case k.
• Why add a capital "F" to all capacitors, but no "Ohm" for resistors?
• GND pin for Rf module F1 seems to be stacked, (but stacked pins not hidden).  but you unstacked the pins for the uC?
• RefDes has standardized abbreviations. F is for fuses. https://en.wikipedia.org/wiki/Reference_designator
• I would prefer a few more Power and GND pins on the generic I/O connector.
• It looks like "VBUS" is not connected to: "VBUS (+5V)" (Both have a PWR_FLAG) In KiCad V8 the power symbol name determines the net name, and thus connections.
• I always prefer some kind of inductor or choke between the power input connector and the power regulator.

Thanks for everyone's replies.

Luckily I fixed 1, 3, and 19 already.

2, Application note AN5165 says there is no need.
5, The values are there, just hidden because of space.
6, I see everyone creating separate pins for programming/debugging, I don't get it. I just see it as a waste of space.
9, It's according to application note AN5165.
12, It will be a really small board, if need be I'll add them.
18, That's the default symbol, I thought of unstacking them but there are like 4 ground pins.

The rest is preference/non-critical.